Cadence® system design and verification solutions, integrated under our Verification Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
More Support Log In
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
The Cadence Academic Network helps build strong relationships between academia and industry, and promotes the proliferation of leading-edge technologies and methodologies at universities renowned for their engineering and design excellence.
Participate in CDNLive
A huge knowledge exchange platform for academia to network with industry. We are looking for academic speakers to talk about their research to the industry attendees at the Academic Track at CDNLive EMEA and Silicon Valley.
Come & Meet Us @ Events
A huge knowledge exchange platform for academia. We are looking for academic speakers to talk about their research to industry attendees.
Americas University Software Program
Join the 250+ qualified Americas member universities who have already incorporated Cadence EDA software into their classrooms and academic research projects.
EMEA University Software Program
In EMEA, Cadence works with EUROPRACTICE to ensure cost-effective availability of our extensive electronic design automation (EDA) tools for non-commercial activities.
Apply Now For Jobs
If you are a recent college graduate or a student looking for internship. Visit our exclusive job search page for interns and recent college graduate jobs.
Cadence is a Great Place to do great work
Learn more about our internship program and visit our careers page to do meaningful work and make a great impact.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
Overview All Courses Asia Pacific EMEANorth America
Instructor-led training [ILT] are live classes that are offered in our state-of-the-art classrooms at our worldwide training centers, at your site, or as a Virtual classroom.
Online Training is delivered over the web to let you proceed at your own pace, anytime and anywhere.
Exchange ideas, news, technical information, and best practices.
The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information.
It's not all about the technology. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
You can do this but you need a PCB Editor Performance license to do it. Bascially schedule the net then using Constraint Manager create pin pairs of the net. Once this is done the pin pair groups are visible in Constraint Manager Physical Tab. You can assign a different PCSET to the different pin pairs.
In reply to steve:
I am using Allegro PCB Design XL 16.3S017 and I was able to schedule the nets, create the pin pairs of the net in the Physical tab, and assigned different PCSETs to each pin pair with my license. Do I still need the PCB Editor Performance license for it to perform a DRC on the physical constraints for pin pairs?
In reply to jackg23:
I've had success with the DRC's correctly showing errors and using PCSets for Pin Pairs. Make sure that after updating the Constraint Manager (CS) that you do a DRC udpate.
I am having some problems with routing, though. When routing traces (manually) between two pins of a pin pair, the line width always defaults to the NET line width, not the Pin Pair line width defined in the CS. The line width in the options control box shows the correct width, but that is not what is drawn. Then, I get a DRC that says the neck length is too long. I'm assuming that this is because the tool does not know which pair of pins I'm connecting until after the trace is completed. Does anyone know how to make the line width default to what is in the constraints manager?
In reply to Brando:
>>When routing traces (manually) between two pins of a pin pair, the line
width always defaults to the NET line width, not the Pin Pair line width
defined in the CS
Thereis was a bug - ensure that you've got the latest hotfix installed.
The pin-pair works nicely, but what if you dont have the luxury of having a pin to schedule. What if you need to connecto the sense line to the force line at a via or to the actual trace of the force line?
In reply to Jonah Stephenson:
I would create a pin pair for the force line and
leave the sense line as default. You can connect the sense line anywhere
on the force line or to a via and the width would not be the same as the pin pair constraint width.
Thanks Brando. I tried creating a pin pair between the force resource line and the DUT pin, and not creating a pair for the sense pin (leaving it as default). When I grab the force pin to in route mode it default to the Min line width of the net, not the Min of the pin pair. What am I doing wrong? The line width in the router shows I want 30 (the value I asigned to the force pin pair) when I grab the pin it only shows the route at 6 (default value).
That was actually my problem also. See the above reply from KHurana. I haven't installed the latest hotfix yet (waiting on the tools admin), but the release notes do address this issue. In the mean time, if I see a line width in the options control box that is different than the default, I just type over that value and then the line width is correct.
I will check that there is a newest hotfix, but I do believe my compay has the latest releases. Do you know that date of the latest hotfis release? Thank you for all your help!
It looks like it was fixed in hotfix 021 which was release 12-10-2010.
Look at item number 846352 of the README_CCR.txt:
846352 ALLEGRO_EDITOR DRC_CONSTR Route connect does not select the pin-pair width for routing.